SOLIDWORKS Hole Wizard with Circular Sketch Pattern

Say you want to add multiple holes in a Hole Wizard feature.  Typically you would add multiple points from the Positions tab and add dimensions/relations.  You can use Linear and Circular Sketch Patterns to create the extra points.

SOLIDWORKS Hole Wizard with Circular Sketch Pattern

In most cases it would be simpler to add a single hole in the Hole Wizard and then use the Linear or Circular FEATURE Pattern.  This can help keep things simpler as a Hole Wizard sketch with many points and relations can be confusing and slower.  Also editing the Sketch Patterns are not as straight forward as you need to right-click on one of the points and “Edit Linear/Circular Pattern”

But if you’ve tried using the Circular Sketch Pattern you may notice it adds an extra point in the center.

SOLIDWORKS Hole Wizard – Adds Extra Point in Center of Circular Pattern

This is actually because there is no dimension for the radius of the circular pattern.  The 4.00 dimension only controls the location of the first point.  The extra point in the center is used to rotate and control the radius.

SOLIDWORKS Hole Wizard – Center Point allows Control of Location and Radius of Center-point

To avoid the extra point in the center, when you create the Circular Sketch Pattern, enable the option ‘Dimension Radius’.  This adds a Construction Line and Radius dimension without adding the center-point.  No more point in the middle!  But you’ll still need to control the angle of the construction line (for example add a vertical relation).

SOLIDWORKS Hole Wizard – Dimension Radius option in Circular Sketch Pattern

Notice the original 4.00 dimension is not actually required if you make the end of the construction line coincident to the origin.

SOLIDWORKS Hole Wizard – Adds Radius Dimension and Construction Line